How are you positioning the head to do that. If the head is mounted longitudinally in the X axis, the how can you interpolate a radius in the Y axis, using a G02 or G03 interpolation in the Z axis, without at least 20 interpolations per stand? That is figuring on a 1 inch wide stand with a .050" stepover per interpolation, which still won't give that great of a finish, imho. And, it's going to take the same amount of time????? Maybe I can learn something new here, and hopefully I can.
Logic would dictate this would be machined at the same time the top of the pedestal is machined and the shaft mounting holes are drilled and tapped. You could make the arc in the z axis or simply move the cutter in the z and y axis and cut moving in the x direction which would be easier on the machine because its not rapidly changing direction in the z at the bottom of the radius. I haven't programed manually writing G code since college, its far too time consuming and risky when programming complex contours and surfaces like what is found on molds. The code is created by the CAM software based on what type of machining strategies you asking it to use whether that be High Efficiency Machining, High Speed Machining or multiple other more conventional guidelines the software will use to create 3D tool path. The crossover is determined by multiple factors including cutter size and the amount of surface deviation allowed by tolerance settings in the software. Many 3d models generated by cad software end up creating surfaces using nurbs rather than lines and arcs making G02 and G03 non existent.
A big cutter turning slow feeding slow vs a small cutter turning tens of thousands of rpm and moving at a much higher feed rate could yield similar machine time, way better finish, more accuracy, and ability to adjust if needed.
Also, if an approximately .150" deep roughing cut, in aluminum, is deflecting a 7/8" ball mill, in a modern CNC, something is wrong. And then there is a .020" spring pass to clean it up. It better not deflect there, even with a dulling cutter, And, you have modern coolants/lubricants to maximize tool wear, and provide a great finish. I find it hard to think an interpolation is the way to go. But, I'm sure I'm missing some considerations, so if I can learn a new, better way, I'm the better for it.
Spring pass indicates same tool path, .020" would be a finish pass but would likely have better results than a true spring pass. It will almost certainly deflect on the .15" cut although the .020" pass would clean up the minor deflection. It will fail to cut as well in the middle where the flutes come together vs the shoulders of the cutter because the feed and speed is so different for the creating a vastly different chip load on the edges of the cutter vs the center where the diameter is effectively much smaller.
A single pass with a finish cut could work but in a production environment it is not most effective or versatile. How will you change the size of your radius if its off with one pass? With a 3D toolpath its a simple adjustment. How much more does a 7/8" solid carbide ball mill cost than a 3/8" or 1/2"? What are you going to do with them when they get dull? You cant sharpen them and use them in the future because they will be too small, but using 3D toolpath you just adjust the size of the cutter in the machine or the program.
As a side note, I used to machine ball bearing bores in racing manual transmissions and was not allowed to interpolate those bores. If caught doing that, I was assured I would be shown the door. We could only cut them with a boring head. The reason was because interpolation still uses a point-to-point toolpath, and is not a true radius like could be achieved by using a boring head. The trans were built for NASCAR, so it had to be some of the most nit-picky stuff I have ever seen short of the aerospace industry and NASA.
That is a totally different application in comparison to what we are talking about and the boring head is the best way to achieve perfectly round holes. As I said in my previous post the ultimate way to finish that would be with a boring or honing operation, but that would take some doing with the half round interrupted cut aspect and long reach required. High quality VMC's that isn't worn can machine round within .0002" pretty easy and cheap machines can hold .0005", but that is due to the machine changing directions 4 times while machining said circle. That being said locational accuracy will typically be better with an interpolated hole vs a boring head due to the backlash being distributed throughout the 4 quadrants of the cut. If you ran your toolpath longitudinal in the groove there is no directional changes in the saddle.
With todays machines its easy to machine 2 separate large blocks of steel with a complex contoured parting lines mirroring each other on a plastic injection mold and have them match and seal off within .001".
That being said how are your shims and hold downs in your kits made? are they not machined in a cnc mill that is interpolating the moon like shape? Or do you have concave and convex form cutters made to create those shapes?